Verification and Validation of Turbulent Flow around a Clark-Y Airfoil

53 Pages·2014·2.59 MB·English

by  Timur Dogan

Verification and Validation of Turbulent Flow around
a Clark-Y Airfoil

58:160 Intermediate Mechanics of Fluids
CFD LAB 2

By Timur Dogan, Michael Conger, Maysam Mousaviraad, Tao Xing and Fred Stern
IIHR-Hydroscience & Engineering
The University of Iowa
C. Maxwell Stanley Hydraulics Laboratory
Iowa City, IA 52242-1585

1. Purpose

The Purpose of CFD Lab 2 is to simulate turbulent airfoil flows following “CFD process” by an
interactive step-by-step approach and to conduct verifications. Students will have “hands-on”
experiences using ANSYS to conducting verification for lift coefficient and pressure coefficient
distributions, and validation for pressure coefficient distribution, including effect of numerical
scheme. Students will manually generate C type mesh and investigate the effect of domain size
and effect of angle of attack on simulation results. Students will analyze the differences between
CFD and EFD, analyze possible sources of errors, and present results in a CFD Lab report.

Geometry Physics Mesh Solution Results
Airfoil (ANSYS General (ANSYS Structured Solution Plots (ANSYS
Design Modeler) Fluent - Setup) (ANSYS Mesh) Methods Fluent- Results)
(ANSYS Fluent -
C-Domain Model (ANSYS Solution)
(ANSYS Design Fluent - Setup) Graphics and
Modeler) Non-uniform Animations
Boundary (ANSYS Mesh) Solution Controls (ANSYS Fluent-
Conditions (ANSYS Fluent - Results)
O-Domain (ANSYS Fluent - Solution)
(ANSYS Design
Setup)

Modeler)
Monitors
Reference Values (ANSYS Fluent -
(ANSYS Fluent - Solution)
Setup)
Turbulent Solution
Solution Initialization
Initialization (ANSYS Fluent -
(ANSYS Fluent - Solution)
Solution)
Run Calculation
(ANSYS Fluent -
Solution)

Flow Chart for “CFD Process” for airfoil flow
2. Simulation Design

The problem to be solved is that of turbulent flows around a Clark-Y airfoil. Reynolds number is
143,000 based on the inlet velocity and airfoil chord length. The following figures show the
illustrations for C type and O type domains. (Note: the figures are not in the exact scale as the
true size of the domain and airfoil).

Table 1 - Main particulars
Parameter Symbol Unit O-type C-Type
Chord Length C m 0.3048 0.3048
Downstream length Lo m - 5
Radius Rc m 5,4,3,2,1 5
Angle of attack α degree 0,6 0

Figure 1 – C and O domain shapes and boundary conditions

In CFD Lab 2, Boundary conditions for C type of mesh will be “inlet”, “outlet”, “symmetry” and
“airfoil”, as described later. Boundary conditions for O type of meshes will be “inlet”, “outlet”,
and “airfoil”. Uniform flow was specified at inlet. For outlet, zero gradients are fixed for all
velocities and pressure is constant. No-slip boundary condition will be used on the “airfoil”.
Symmetric boundary condition will be applied on the “symmetry”. The meshes and the
simulations that will be conducted are shown in Tables 2 and 3 respectively.
Table 2 - Mesh
Domain Radius Angle of Attack (AOA)
Mesh Name
Type [m] [degree]
C-mesh C
fine
medium 5
coarse
Domain-R5 0
Domain-R4 O 4
Domain-R3 3
Domain-R2 2
Domain-R1 1
AOA6 5 6

Table 3 - Simulation Matrix
Study Mesh
Domain size Domain-R1, Domain-R2, Domain-R3, Domain-R4, Domain-R1
V&V and effect of
fine, medium, O-coarse
numerical scheme
Domain shape C-mesh
Angle of attack AOA6

All EFD data and CFD materials for turbulent airfoil flow in this Lab can be downloaded from
class website (http://www.engineering.uiowa.edu/~me_160/).
3. ANSYS Workbench

3.1. Start > All Programs > ANSYS 15.0 > Workbench 15.0

3.2. Toolbox > Component Systems. Drag and drop Geometry, Mesh and Fluent
components to Project Schematic and name components as per below. Create

connection as per below.
3.3. File > Save As…. Save project on the H: drive. Name the file “CFD Lab 2”.

4. Geometry

4.1. From the Project Schematic, right click on the C-Domain Geometry and select New
Geometry…

4.2. Make sure that Unit is set to Meter (default value).
4.3. Go to the class website and download Airfoil geometry (You can download the file by
right clicking and selecting save as).

4.4. File > Import External Geometry File… Select intro-airfoil.igs and click Open. Click
Generate.

4.5. Add a new plane by selecting the New Plane button. For the Type select From Point
and Normal.
4.6. For the Base Point, zoom in and select the point at the trailing edge as seen below.

4.7. For the Normal Defined By, select the XYPlane on the Tree Outline. Then click
Generate. This creates a plane with the origin at the trailing edge point.

4.8. Make sure the plane you just created is selected under tree outline then click the New
Sketch button.
4.9. In Sketching Toolboxes>Constraints, Enable the Auto Constraints option to pick the
exact point as below

4.10. Sketching > Arc by Center. Draw an arc centered at the trailing edge origin as
per below. Make sure the end points are on the y-axis.

4.11. Sketching > Rectangle by 3 Points. Draw a rectangle as per below.
4.12. Dimensions > General. Size the arc and rectangle with a radius of 5m and a
width of 5m respectively as seen below.
4.13. Delete the line that makes the left side of the rectangle by selecting it and pressing
Delete on the keyboard.

4.14. Concept > Surface from Sketches. Select the sketch you just made under tree
outline, click Apply then click Generate.